The loading and solution phase starts with the /SOLU command. In this phase, you do the following tasks:
Other solution-related items - master DOF and gap conditions - are also defined in this phase.
Analysis types are generic and independent of discipline:
On menu mode, control panels are available to define analysis type and analysis options. For non-menu mode, ANTYPE command replaces KAN.
ANTYPE, STATIC (or 0)
TRANS (or 4)
MODAL (or 2)
etc.
MODOPT ! Modal analysis options TRNOPT ! Transient analysis options HROPT ! Harmonic analysis options BUCOPT ! Buckling analysis options SSTIF ! Stress stiffening NROPT ! Newton-Raphson options Etc.
Preconditioned Conjugate Gradient (PCG) solver has been added as an alternate to the default frontal solver. The PCG solver requires less file space but more memory than other solvers and is faster for larger models(wavefronts > 1000). PCG is well-suited for problems with very large, sparse, symmetric matrices, such as those encountered in magnetic field analysis.
/SOLUTION ANTYPE,STATIC EQSLV,PCG . . . . . . . .
There are six categories of loads, each with a generic set of commands:
Family Category D ! DOF Constraints (displacements,temperatures,...) F ! "FORCES" (forces,moments,heatflows,...) SF ! Surface Loads (pressures,convections,...) BF ! Body Loads (temperatures,heat generations,...) ACEL ! Inertia Loads (accelerations,...) LDREAD ! Coupled-Field Loads (thermal strain,...)
DOF constraints available in each discipline:
Discipline Degree of Freedom ANSYS Label
Structural Translations UX,UY,UZ
Rotations ROTX,ROTY,ROTZ
Thermal Temperature TEMP
Magnetic Vector Potential AX,AY,AZ
Scalar Potential MAG
Electric Voltage VOLT
Fluid Velocities VX,VY,VZ
Pressure PRES
Turb. Kinetic Energy ENKE
Turb. Dissipa. Rate ENDS
DOF constraint commands:
Location Commands Nodes D,DSYMM,DLIST,DDELE,DSCALE,DCUM Keypoints DK,DKLIST,DKDELE Lines DL,DLLIST,DLDELE Areas DA,DALIST,DADELE Transfer DTRAN,SBCTRAN
"FORCE" available in each discipline:
Discipline "Force" ANSYS Label
Structural Forces FX,FY,FZ
Moments MX,MY,MZ
Thermal Heat Flow Rate HEAT
Magnetic Current Segments CSGX,CSGY,CSGZ
Magnetic Flux FLUX
Electric Current AMPS
Fluid Fluid Flow Rate FLOW
Heat Flow Rate HEAT
"FORCE" load commands:
Location Commands Nodes F,FLIST,FDELE,FSCALE,FCUM Keypoints FK,FKLIST,FKDELE Transfer FTRAN,SBCTRAN
Surface loads available in each discipline:
Discipline Surface Load ANSYS Label
Structural Pressure PRES
Thermal Convection CONV
Heat Flux HFLUX
Magnetic Maxwell Surface MXWF
Electric -none- -none-
Fluid Fluid-Structural FSI
Impedance IMPD
Convection CONV
Heat Flux HFLUX
All Superelement SELV
Load Vector
Surface load commands:
Location Commands
Nodes SF,SFLIST,SFDELE,SFSCALE,SFCUM,SFFUN,
SFGRAD
Elements SFE,SFELIS,SFEDEL,SFBEAM,SFFUN,SFGRAD
Lines SFL,SFLLIST,SFLDELE,SFGRAD
Areas SFA,SFALIST,SFADELE,SFGRAD
Transfer SFTRAN,SBCTRAN
e.g. NSEL,...
SF,ALL,PRES,5000 ! Pressure on all selected nodes
Body loads available in each discipline
Discipline Body Load ANSYS Label
Structural Temperature TEMP
Fluence FLUE
Thermal Heat Generation Rate HGEN
Magnetic Current Density JS
Virtual Displacement MVDI
Electric -none- -none-
Fluid Heat Generation rate HGEN
Body load commands:
Location Commands Nodes BF,BFLIST,BFDELE,BFSCALE,BFCUM,BFUNIF Elemnets BFE,BFELIS,BFEDEL,BFESCAL,BFECUM Keypoints BFK,BFKLIST,BFKDELE
Inertia load commands are the same as at Revision 4.4.:
ACEL,OMEGA,DOMEGA,CGLOC,CGOMEGA,DCGOMG,IRLF
Coupled-field loads are applied using the new command LDREAD which reads data from the results file and applies them as loads. For example,
LDREAD,TEMP,,,5.78,,,THERMAL,RTHreads temperature at time=5.78 from file THERMAL.RTH.
Applied loads may be displayed with the following three commands:
/PBC ! For Ds and Fs /PSF ! For SFs /PBF ! For BFs
For examples:
/PBC,U,,1 ! For displacements /PBC,F,,1 ! For forces /PBC,all,,a ! For all appropriate symbols /PBC,ACEL,,1 ! Applied accelerations /PSF,PRES,NORM,1 /PBF,TEMP,,1
SOLVE is the command that initiates the solution; it reads data from database to calculate solution and writes results to database and also to the results file.
This is the actual computing portion of the analysis, and a complex ANSYS job often requires considerable amount of CPU time. It is advisable that you save the database prior to executing the SOLVE command ( with "SAVE, filename,db") and exit the ANSYS program. Next, create a batch submit file as the following:
# @$-lt 20:00 # @$-lw 32mb # @$-eo # @$-me ANSYS <<'EOT' /BATCH /RESUME,<Filename>,db /SOLUTION SOLVE FINISH EXIT 'EOT'This batch job can then be submitted to the tiber with the "qsub" command:
qsub batch-submit-file-name
The IBM RS6000 cluster machines are to be used as back-end machines, though users can login to the hudson and interactively run ANSYS. Users are requested to run ANSYS interactively only for preparing the ANSYS commands in /PREP7 and for reviewing the results in /POST1 or /POST26. The CPU intensive solution phase must be run in batch mode. If users abuse the trust and run the CPU intensive solution phase that makes hudson unavailable to other users, severe restrictions will be imposed to all ANSYS users. As a rule of thumb, if the SOLVE takes more than 3 minutes of CPU time, run it in batch.
Two of the RS6000s, snake and pecos, have been designated to run ANSYS batch jobs. The total size of files created by ANSYS cannot exceed 2 GB in /tmp in pecos, while it is possible to exceed 2 GB in snake by assigning files to two directories, /tmp and /wrk. Thus an ANSYS job that may create a total file size greater than 2 GB must run on snake. Users may follow the examples below to prepare an ANSYS batch script file on the hudson and submit it to the pecos or the snake by the qsub command with "-q ANSYS" or "-q ANSYS.snake". The ANSYS queue will run ANSYS on either pecos or snake, while ANSYS.snake will run ANSYS only on snake.
qsub -q ANSYS .
qsub -q ANSYS.snake .
The script file and ANSYS input file may be kept in your home directory
or its subdirectory.
#@$-lt 20:00
#@$-lw 32mb
#@$-eo
#@$-me
date
mkdir /tmp/tang
cd /tmp/tang
cp /user/marge/spring* .
/usr/local/bin/ANSYS <<'EOT'
/BATCH
! /assign,tri,spring,tri,/wrk/tang/ !!! Only for ANSYS.snake with
! /assign,emat,spring,emat,/wrk/tang/ !!! total file size > 2 GBs
/input,spring,prep
/input,spring,ldso
/input,spring,post
/input,spring,opt
/input,spring,full
/exit
'EOT'
ls -l /tmp/tang !!! Check files created created by ANSYS
! ls -l /wrk/tang !!! On snake only
mv *.rst /tiber/support/tang/ANSYS/.
mv *.db /tiber/support/tang/ANSYS/.
rm /tmp/tang/* !!! Clean up your files to provide file space
! rm /wrk/tang/* !!! for next job to use.
The ANSYS program creates several output files that are in the order of tens of megabytes in pecos temporary file space. These files are not interactively accessible because pecos is not directly accessible to user, but users can use rsh command to browse these files:
rsh pecos ls -l /tmp/usrname rsh pecos cat /tmp/usrname/filename.out rsh pecos rm /tmp/usrname/xx.To copy a file from /tmp/usrname on pecos to somewhere in your tiber directory, you need to have hudson.nist.gov in your tiber .rhosts and then use:
rcp pecos:/tmp/usrname/xx subdir/xxIf your home directory is on hudson and the file is too large to keep on hudson, specify a full pathname to your tiber directory:
rcp pecos:/tmp/marge/xx /tiber/nist/marge/xx
Multiple load steps can be solved by three methods:
... Load data LSWRITE ----> File.S01 ! Load data LSWRITE ----> File.S02 ! Load data LSWRITE ----> File.S03 ! ... LSSOLVE
New LSCLEAR command clears loads and load step options in the database, while LSREAD and LSDELE reads and deletes a load step file, respectively.
With the array parameter method, array parameters of type TABLE are used to define load versus time:
*DIM,LOAD,TABLE,5 LOAD(1)=0.0,560.0,560.0,238.5,0.0 LOAD(1,0)=0.0,0.8,7.2,8.5,9.3Then use a do-loop to apply the load and solve it:
DTIME=0.01 ! Time step size
*DO,TIMEV,1.0E-6,5.8,DTIME
TIME,TIMEV
F,293,FY,LOAD(TIMEV)
SOLVE
*ENDDO
The multiple SOLVE method defines load data, issues SOLVE; changes load
data, issues SOLVE; and so on. This method is better suited for batch
mode than for interactive mode.
New output controls separate print and post:
OUTPR,Item,FREQ,..... OUTRES,Item,FREQ,....If you have already prepared an ANSYS input file with PREP7, at the system prompt, you can redirect the input file to ANSYS and run it in the background mode:
ANSYSoutput-file-name &, or /input,input-file-name,ext,dir within ANSYS.
/SOLU ! Enter the SOLUTION processor
ANTYPE,STATIC ! Static (steady-state) analysis
TUNIF,0 ! Initial Uniform Temp = 0
KBC,1 ! Step loading
CNVTOL,TEMP,1.0,1.0E-6
CNVTOL,HEAT,1.0,1.0E-6
/FORMAT,,E,14,6
PI=3.1415927
NSEL,S,,,91,95 ! Select node 91-95, Y=4.0-4.2
F,ALL,HEAT,10/PI ! Constant heat flow rate per radian
! Total heat load = 10000 nW
NSEL,S,LOC,Y,-3.5
D,ALL,TEMP,0 ! Base Temperature
ALLSEL
OUTPR,NSOL,1
OUTRES,NSOL,1 ! Write node solutions to the result file
/PBC,HEAT,1 ! Show heat rate load
/PBC,TEMP,1 ! Show boundary temp load
EPLOT
AUTOTS,OFF ! Turn off automatic load-stepping
NSUBST,20 ! Only 1 substep is sufficient
SOLVE
SAVE
FINISH ! End of SOLUTION process
/POST1 ! Enter postprocess
* ASK,LS,'Load Step to Display LS:',1
SET,LS,LAST
/TITLE,TEMPERATURE CONTOUR PLOT
NSEL,S,,,1,150
PLNSOL,TEMP ! Display temperature
/SOLUTION ! Enter the SOLUTION processor
ANTYPE,TRANS ! Set analysis type = transient
TUNIF,0 ! Initially uniform temp = 0
TIMINT,ON ! Transient effect considered
KBC,1 ! Step loading
/FORMAT,,E,14,6
PI=3.1415927
TIME,100 ! Total of 100 sec
DELTIME,600 ! What does it mean?
AUTOTS,OFF ! Turn off automatic load-stepping
NSUBST,400 ! Use 400 substeps - 4 steps per sec
NSEL,S,,,91,95 ! Select node 91-95, i.e., Y = 4.0 - 4.2
F,ALL,HEAT,10.0/PI ! Constant heat flow rate per radian
! Total of 10000 nW applied
NSEL,S,LOC,Y,-3.5
D,ALL,TEMP,0
ALLSEL
/PBC,HEAT,1 ! Show heat load
/PBC,TEMP,1 ! Show temperature load
EPLOT
OUTPR,NSOL,4
OUTRES,NSOL,4 ! Write all solutions to the result file
*DO,TIMEVAL,BGNTIME,ENDTIME,DELTIME
TIME,TIMEVAL
SOLVE
*ENDDO
FINISH ! End of SOLUTION process
*ASK,LS,'Load Step to Display LS:',1
SET,LS,LAST
/POST26 ! Enter postprocess time history
/TITLE,TEMPERATURE CONTOUR PLOT
PLNSOL,TEMP ! Display temperature
NSOL,2,1,TEMP,Node-1
NSOL,3,11,TEMP,Node-11
NSOL,4,41,TEMP,Node-41
NSOL,5,71,TEMP,Node-71
NSOL,6,91,TEMP,Node-91
NSOL,7,101,TEMP,Node-101
PRNSOL,2,3,4,5